
[Sponsors] 
January 30, 2014, 08:40 
Confuse about Nu Number in Laminar Flow

#1 
Senior Member
Join Date: Jan 2011
Posts: 236
Rep Power: 9 
Hi I did simple heat transfer problem of flow throw a circular pipe with constant heat flux at wall. Usually for laminar flow with constant heat flux the Nusselt Number should be 4.36 ? when I view surface nusselt number from Report>Wall Fluxes>Surface Nusselt number it give me Nusslet number as 11.61 ? Why this deffer from the theortical value as (4.36)?
Mariam 

January 30, 2014, 08:54 

#2 
New Member
Smith
Join Date: Jan 2014
Posts: 9
Rep Power: 5 
dear mariam and sara,
In fact FLUENT compute h (heat transfer coefficient) and NU number wrong and you should compute them manually as follows: h=mdat*cp*(TwallTbulk) Nu=hD/k Sincerely 

January 30, 2014, 08:59 

#3 
Senior Member
Join Date: Jan 2011
Posts: 236
Rep Power: 9 
Hi Alek thanks a lot for the quick respond. You mentioned in your relation Twall & Tbulk? the problem I not have both of these temperatures because I used fixed heat flux at the wall not fixed wall temperature? So how I can predict Twall in this case?


January 30, 2014, 09:23 

#4 
New Member
Smith
Join Date: Jan 2014
Posts: 9
Rep Power: 5 
The Twall which is computed with FLUENT is right and you can use it.


January 30, 2014, 09:25 

#5 
Senior Member
Join Date: Jan 2011
Posts: 236
Rep Power: 9 
Do you mean I need to plot Twall along the wall? what about Tbulk how i can compute it?


January 30, 2014, 09:27 

#6 
New Member
Smith
Join Date: Jan 2014
Posts: 9
Rep Power: 5 
If you send me an email I can send you a good document.


January 30, 2014, 10:33 

#7  
Senior Member
François Grégoire
Join Date: Jan 2010
Location: Laval University, Canada
Posts: 387
Rep Power: 10 
Quote:
Fluent calculates the heat transfert coefficient (h) from various correlations depending on the physics. It's your homework to verify in the Theory Guide which correlation Fluent uses according to the physics of your model, then decide if you should modify it or not. Last edited by macfly; January 30, 2014 at 12:00. 

January 30, 2014, 11:44 

#8 
Senior Member
Join Date: Jan 2011
Posts: 236
Rep Power: 9 
Hi Macfly I not have problem with the theory. I tried solve problem with constant heat flux at a cylinder wall with laminar flow case it must give me Nu=4.36 but it give different value? I am not one of fluent designer to know how FLUENT predict Nu values you answer is vague to me?


January 30, 2014, 12:08 

#9  
Senior Member
François Grégoire
Join Date: Jan 2010
Location: Laval University, Canada
Posts: 387
Rep Power: 10 
Quote:
 maybe your mesh is not fine enough?  maybe the flow is not fully developped? What I'm saying wouldn't sound vague if you took a look at the theory guide in order to understand what Fluent is doing. I guess you're doing some engineering homework and you have to put some thinking into it. You don't become an engineer just clicking on buttons expecting to get the right number on the output. 

January 30, 2014, 12:19 

#10 
New Member
Smith
Join Date: Jan 2014
Posts: 9
Rep Power: 5 
Dear maryam and Sara
you can use the following relations to compute h and NU manually: Q=q''Px=mdat*C*(Tbulk,xTbulk,in)>Tbulk,x=(q''Px/mdat*C)+Tbulk,in h(x)=q''/(TwallTbulk,x) Twall is calculated by Fluent 

February 9, 2014, 02:12 
How to make inlet velocity fixed along a pipe

#11 
Senior Member
Join Date: Jan 2011
Posts: 236
Rep Power: 9 
Hello
I have a query to how i can make the inlet velocity value fixed from pipe inlet until pipe outlet? is that possible in Fluent? knowing that the flow is laminar? 

July 28, 2015, 11:41 

#12 
Senior Member
Daniele
Join Date: Oct 2010
Location: Italy
Posts: 995
Rep Power: 17 
Question is not very clear to me; do you mean have a fully developed flow so to have a constant velocity profile?
If so, just use periodic boundary condition.
__________________
Google is your friend and the same for the search button! 

July 29, 2015, 03:28 

#13 
Senior Member
Join Date: Jan 2011
Posts: 236
Rep Power: 9 
Hi ghost if I want fully developed flow I can use periodic boundary by defining inlet as periodic boundary?? I need to know how to use periodic boundary??
mariam 

July 29, 2015, 03:43 

#14 
Senior Member
Daniele
Join Date: Oct 2010
Location: Italy
Posts: 995
Rep Power: 17 
Yes, just change the inlet/outlet to periodic.
Then in periodic settings set the pressure gradient or mass flow rate.
__________________
Google is your friend and the same for the search button! 

July 29, 2015, 04:47 

#15 
Senior Member
Daniele
Join Date: Oct 2010
Location: Italy
Posts: 995
Rep Power: 17 
The main problem is how the heat transfer coefficient (h) is defined: as you know there is bulk temperature into the equation, but what is bulk temperature?
Adjacent cell to the wall? Or temperature on the axis? Or....? For each defined bulk temperature you will obviously obtain different values of h, and so different values of Nusselt number. Related to your problem (fluid flow in pipe, laminar, with constant heat flux) I suggest to: 1 Draw 2D axisymmetric pipe 2 Set a periodic translational pipe 3 Enable energy equation, but disable in solution controls the energy equation (1 step: solve the momentum equation) 4 Once the velocity field is converged, eneable energy equation and disable momentum equation (2 step: solve the enrgy equation) 5 Create a line in y direction at a predefined x location (in the middle of the pipe for example) 6 Go to Reports>surface integrals>area weight average: select temperature and the line you created (This will be the mixed mean temperature, n other words Tbulk) 7 Evaluate the temperature on the wall, at the line you created 8 Calculate h as h=Q/(TwallTbulk), where Q is your heat flux (Watt/m2). 9 Evaluate Nusselt as Nu=h*D/k, where D is pipe diameter (m), k thermal conductivity (W/m/K) This should give you a good approximation.
__________________
Google is your friend and the same for the search button! 

July 29, 2015, 05:04 

#16 
Senior Member
Join Date: Jan 2011
Posts: 236
Rep Power: 9 
really thanks ghost82 for the valuable illustration. I will told you what I did, I run my case as described previously it converged and the contours of temperature is quite good when compared to the literature. I want now to predict h & Nu at a distance (0.69825 m) from the pipe inlet hence I draw a vertical line at this distance I evaluate Tbulk and used surface integral>area weighted average along the line Tb=298.6429 K then evaluated Tw at the wall which be 308.17706 K now I predict h from the relation knowing that heat flux at the wall is 8846.4 W/m^2 as below:
h=8846.4/(TwTb)=8846.4/(308.17706298.6429)=927.8635978 W/m^2.K this value is higher than that predicted from experiments which is 888 W/m^2.K?? I can sent you my case file and the paper I compare with if you want have a look? Thanks mariam 

July 29, 2015, 05:09 

#17 
Senior Member
Join Date: Jan 2011
Posts: 236
Rep Power: 9 
I forgot to mention my case not fully developed from inlet it a startup flow which be fully developed at the end pipe section only. So i think I do not need for periodic boundaries.


July 29, 2015, 05:12 

#18  
Senior Member
Daniele
Join Date: Oct 2010
Location: Italy
Posts: 995
Rep Power: 17 
Quote:
Send me the paper; I think that 927 vs. 888 should be acceptable, it's a 4% "error", I don't know.. Moreover: are you sure your simulation reflects 100% the experimental setup? Daniele
__________________
Google is your friend and the same for the search button! Last edited by ghost82; July 29, 2015 at 15:24. 

July 30, 2015, 11:04 

#19 
Senior Member
Daniele
Join Date: Oct 2010
Location: Italy
Posts: 995
Rep Power: 17 
Just to make public my thoughs I wrote you by email:
I think Tbulk could be calculated better by massweightedaverage and not areaweightedaverage. Moreover, Book "Fundamentals of heat and mass transfer" by Incropera defines a Tm (Tbulk), as in the attached picture. I think you can create a custom field function named for example numerator: density*axialvelocity*specificheatcp*temperature Then evaluate the integral on the radial line you defined: Reports>Surface integrals>Integral and choose Custom field function>numerator Then divide this number by the (mass flow rate*cp). Mass flow rate can be obtained in reports>fluxes. If your cp is a function of temperature you can evaluate an average cp by massweightedaverage. Results of Tm should be similar to Tbulk evaluated by massweightedaverage. Daniele
__________________
Google is your friend and the same for the search button! 

November 23, 2015, 15:21 

#20  
New Member
Join Date: Mar 2009
Posts: 14
Rep Power: 9 
Quote:
I realize this thread is a bit old now, but can you explain further what you mean by the above statement? If your case is not fully developed it is not surprising that you would get a higher Nu than the theoretical result for fullydeveloped conditions. The temperature profile is flatter in the developing region, and the difference between the bulk temperature and the wall temperature is smaller than in the fully developed region. For a given fixed wall heat flux, this means h will be higher in the developing region. So it is important to use periodic conditions for temperature, not just velocity. 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
decomposePar pointfield  flying  OpenFOAM Running, Solving & CFD  28  December 30, 2013 16:05 
AMI interDyMFoam for mixer  danny123  OpenFOAM Running, Solving & CFD  4  June 19, 2013 04:49 
parallel code  samiam1000  SU2  3  March 25, 2013 05:55 
Stable boundaries  marcoymarc  CFX  33  March 13, 2013 07:39 
AMI speed performance  danny123  OpenFOAM  19  October 24, 2012 07:44 